View source for VCO Performance Simulations

The following tutorial assumes that you have a voltage controlled oscillator (VCO) with differential outputs already designed and you now wish to find various performance criteria such as phase noise, tuning range, etc.

=Phase Noise=
* Make sure that your tuning voltage is set such that your VCO oscillates at the desired frequency.
* From the Analog Design Environment (ADE) click '''Choose Analysis ...''' and choose '''pss'''
**In the '''Fundamental Tones''' section make sure '''Beat Frequency''' is selected and enter your best guess as to what the frequency of oscillation should be (i.e., enter your desired operating frequency). Make sure that '''Auto Calculate''' is NOT selected.
**In '''Output harmonics''' select '''Number of harmonics''' and enter 10.
**Under '''Accuracy Defaults (errpreset)''' select '''conservative''' and enter the required stabilization time under '''Additional Time for Stabilization (tstab)'''.
***''tstab'' is obtained from a transient simulation. It is the time that it takes for the output of your oscillator to settle to a steady state (in terms of amplitude and frequency).
**Select '''Oscillator''' and then select one of the differential outputs for '''Oscillator node''' and the other differential output for the '''Reference node'''.
**Click '''Apply'''

*Nose select '''pnoise''' analysis in the '''Choosing Analysis''' window
**Set the '''Sweeptype''' to '''relative'''
**Enter 1 for the '''Relative Harmonic'''
**Select '''Start-Stop''' and enter 1 kHz and 100 MHz for the '''Start''' and '''Stop''' frequencies, respectively
**Set the '''Sweep Type''' to '''Logarithmic''' and set the '''Points Per Decade''' to 201
**Under '''Sidebands''' select '''Maximum sideband''' and enter 30
**Set the '''Output''' to '''voltage''' and select one of the differential outputs for the '''Positive Output Node''' and the other differential output for the '''Negative Output Node'''
**Set the '''Input Source''' to none
**Leave the '''Noise Type''' to sources
**Click '''OK'''

*To plot the output, in the ADE Window click '''Results -> Direct Plot -> Main Form ...'''
**Under '''Analysis''' select '''pnoise'''
**Under '''Function''' select '''Phase Noise'''
**Click Plot

=Tuning Range=
*Set your tuning voltage sources to be controlled by a variable (e.g., vtune)
*In the ADE window click on '''Choose Analysis ...'''
**Select '''tran'''
**Set the '''Stop Time''' to an appropriate value that ensures that the output of your VCO has settled and that at least 3/4 of the ''total'' simulation time consists of oscillation with a stable output.
** Set the '''Accuracy Defaults (errpreste)''' to '''conservative'''
**Click '''OK'''

*In the ADE window click '''Tools -> Parametric Analysis'''
**Enter the variable name for the control voltage under '''Variable Name'''
**Set the '''From''' and '''To''' values so that the control voltage is swept from o to Vdd
**Set the '''Total Steps''' to 10
**Click '''Analysis -> Start'''

*To plot the results open up the calculator
**In the calculator (under the ''tran'' tab) click '''vt''' and then select one of the differential outputs of the VCO on the schematic
**In the special functions of the calculator click '''frequency'''
**Click the plot button in the calculator

=Phase Noise vs. Tuning Voltage=
*Set your tuning voltage source to be controlled by a variable (e.g., vtune)
*Use the setup for '''pss''' analysis from the ''Phase Noise'' simulation above
*Configure the '''pnoise''' the same as above too, except select '''Single-Point''' under '''Output Frequency Sweep Range (Hz)''' and enter the offset frequency that you are interested in (e.g., 100 kHz or 1 MHz)
**Everything else should be the same as in the ''Phase Noise'' simulation above
*In the ADE window click '''Tools -> Parametric Analysis'''
**Enter the variable name for the control voltage under '''Variable Name'''
**Set the '''From''' and '''To''' values so that the control voltage is swept from o to Vdd
**Set the '''Total Steps''' to 10
**Click '''Analysis -> Start'''
*To plot the results, in the ADE click '''Results -> Direct Plot -> Main Form ...'''
**Under '''Analysis''' select '''pnoise'''
**Under '''Function''' select '''Phase Noise'''
**Click '''Plot'''

=Amplitude vs. Tuning Voltage=
*Set your tuning voltage source to be controlled by a variable (e.g., vtune)
*In the '''Analog Design Environment''' click on '''Choose Analysis ...'''
**Select '''tran'''
**Set the '''Stop Time''' to a time such that the output of the VCO has settled and steady-state oscillation makes up for at least 1/2 of the ''total'' simulation time
**Set the '''Accuracy Defaults (errpreset)''' to '''conservative'''
**Click '''OK'''
*In the ADE window click '''Tools -> Parametric Analysis'''
**Enter the variable name for the control voltage under '''Variable Name'''
**Set the '''From''' and '''To''' values so that the control voltage is swept from o to Vdd
**Set the '''Total Steps''' to 10
**Click '''Analysis -> Start'''
*To plot the results, open up the calculator
**In the calculator, under the ''tran'' tab, click '''vt''' and select one of the VCO's differential outputs on the schematic
**In the calculator click on the special function '''ymax'''
**Click '''vt''' again and now select the other differential output on the schematic
**In the calculator click on the special function '''ymin'''
**Now click the subtract button ('-')
**Click the plot button in the calculator